SOLIDWORKS Sheet Format FAQ

Article by GoEngineer on Jan 20, 2013

SOLIDWORKS Drawing templates contain all the document specific information that is found in the Tools > Options > Document Properties dialog (i.e. units, standard, fonts, arrow sizes, etc.). SOLIDWORKS Sheet formats contain the Title block information as well as the information from the Sheet Properties dialog. 

When saving a drawing template, the sheet should be empty (even if the sheet format is deleted from the Feature Manager). 

To save a sheet format, when it is displayed go to File > Save Sheet Format. 

How do I get rid of default sheet formats? 

If you do not want to have the default sheet formats available when creating a new drawing, one of the following requirements must be met: 

  1. A new folder must be specified in Tools->Options->File Locations->Sheet Formats AND a .slddrt must reside in this folder (if this folder does not contain a .slddrt file, then the default templates will be used).

    OR

  2. The default sheet format files must be moved from the \data\*.slddrt. 

Where is the setting to control the sheet format/size popup menu? 

The popup dialog of sheet format/size depends on the type of the drawing template. 

  1. If creating a drawing template without a sheet format (i.e. it's a blank sheet) you’ll get the popup dialog when loading this template.
  2. If creating a drawing template with a sheet format, then it is not possible to get the popup dialog when loading this template. 

How do I import a sheet format into SOLIDWORKS from a DWG file? 

Open the DWG file in SOLIDWORKS. Highlight the entities that will make up the sheet format by selecting them using a selection box. Hit CTRL+C to copy the selected entities. Create a new drawing. Right-click in the drawing and select Edit Sheet Format. Delete any existing contents and hit CTRL+V to paste the DWG contents into the SOLIDWORKS sheet format. Go to File > Save Sheet Format and save the sheet format as a .slddrt to be used in other SOLIDWORKS drawings. 

How can a user make a new drawing template that issues a prompt to select a sheet format? 

The drawing template needs to be saved without any sheet format in it. This will cause the user to be prompted to select a sheet format when making a new drawing using that template. To accomplish this, right-click on the Sheet Format in the design tree and select Delete; then save the drawing template. 

How is a drawing created that has different sheet formats for each sheet?

This can be easily achieved by simply changing the sheet format after the sheet has been added to a drawing.

Right-click the Sheet Name in the feature tree, select Properties. In the Sheet Properties dialog, browse to and select the desired alternate sheet format. 

Why is a third angle projection type not retained when saving a sheet format? 

The type of projection and the other sheet properties are not saved in a sheet format; they are saved in an individual drawing file or a drawing template. Sheet formats can store linked custom properties, title block information, anchor points, and OLEs.

Why can't predefined views be saved in a sheet format?

 Predefined views cannot be saved in sheet format. By design, sheet formats cannot hold drawing views. They can only contain sketch entities and annotations.

Can a revision table be saved to a SOLIDWORKS drawing sheet format? 

Unfortunately, a Revision Table cannot be saved to a drawing sheet format. A revision table can only be saved to the Drawing template.

Why is the sheet formats greyed out when creating a new drawing from a part? 

Check Tools->Options->System Options->File Locations->Show Folders for. Sheet Formats and make sure that it is pointing to the location on the hard-drive where the sheet formats are located. 

Where are drawing sheet formats stored? 

The default location for drawing sheet formats is: 

Windows® XP: C:\Documents and Settings\All Users\Application Data\SOLIDWORKS\\lang\sheetformat 

Windows Vista®, Windows® 7: C:\ProgramData\SOLIDWORKS\\lang\sheetformat 

It is possible to change the location, from the main menu -> Tools -> Options -> System Options -> File Locations -> Sheet Formats. 

What causes the message, "The sheet format could not be located." each time a new sheet is added to a drawing? 

A drawing template can be saved with or without a sheet format. A new drawing created from a template that does not include a sheet format will prompt for a sheet format when a new drawing is started. A new drawing which does include a sheet format will simply display the stored sheet format. In this case, when adding a sheet, SOLIDWORKS will search the path where the original sheet format was located when the template was saved. If the sheet format is no longer at that location, then there will be a message when adding new sheets. To correct the problem, re-save the drawing templates with the current sheet format paths or simply remove the sheet format from the template.

A user has a drawing template with a sheet format inside. If a new drawing is opened with this template, and a new sheet is added, the following message appears, "The sheet format could not be found", why? 

To resolve this: 

  1. Open the drawing template file.
  2. From the File menu, select Save Sheet Format, save the sheet format to the default installation directory of sheet formats, for example: C:\ProgramData\SOLIDWORKS\\lang\sheetformat
  3. Right-click on the current sheet, select Properties, browse to a new saved sheet format, select and reload it.
  4. Save the drawing template, and later on, on the same machine, when adding more sheets, the error message should not prompt. 

How can a custom property defined in a part be linked to an annotation in the drawing sheet format? 

To accomplish this, include a drawing view of the model with the desired custom properties. You can then access those properties when creating linked annotations. The drawing view will not be included when you ‘Save Sheet Format’, but the linked annotations will retain the correct source-property information.

More SOLIDWORKS FAQ's 

Corrupted SOLIDWORKS Files FAQ

DraftSight FAQ's

SOLIDWORKS manage Client Install Guide

About GoEngineer

GoEngineer delivers software, technology and expertise that enable companies to unlock design innovation and deliver better products faster. With more than 35 years' experience and tens of thousands of customers in high tech, medical, machine design, energy and other industries, GoEngineer provides best-in-class design solutions from SOLIDWORKS CAD, Stratasys 3D printing, Creaform & Artec 3D scanning, CAMWorks, PLM, Altair, and more

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